Programming Examples - HEIDENHAIN iTNC 530 User Manual

9.11 Programming Examples

Example: Ellipse
Program sequence
The contour of the ellipse is approximated by
many short lines (defined in Q7). The more
calculation steps you define for the lines, the
smoother the curve becomes.
The machining direction can be altered by
changing the entries for the starting and end
angles in the plane:
Clockwise machining direction:
starting angle > end angle
Counterclockwise machining direction:
starting angle < end angle
The tool radius is not taken into account.
%ELLIPSE G71 *
N10 Q1 = +50 *
N20 Q2 = +50 *
N30 Q3 = +50 *
N40 Q4 = +30 *
N50 Q5 = +0 *
N60 Q6 = +360 *
N70 Q7 = +40 *
N80 Q8 = +30 *
N90 Q9 = +5 *
N100 Q10 = +100 *
N110 Q11 = +350 *
N120 Q12 = +2 *
N130 G30 G17 X+0 Y+0 Z-20 *
N140 G31 G90 X+100 Y+100 Z+0 *
N160 T1 G17 S4000 *
N170 G00 G40 G90 Z+250 *
N180 L10.0 *
314
Center in X axis
Center in the Y axis
Semiaxis in X
Semiaxis in Y
Starting angle in the plane
End angle in the plane
Number of calculation steps
Rotational position of the ellipse
Milling depth
Feed rate for plunging
Feed rate for milling
Set-up clearance for pre-positioning
Definition of workpiece blank
Tool call
Retract the tool
Call machining operation
Programming: Q-Parameters